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I have a top level project directory with about 40 Assembly files and several hundred SLDPRT files and they are all highly dependent on each other.

The original version of this works fine and has no errors that we know of. Now I wish to safely clone this entire set of design files to form the basis of the next iteration of our design.

(The originals are of course backed up off-site and are entirely safe from any accidental corruption by stray references in the new cloned version.)

The question is, given the complexity of the project and the huge number of cross-references in the design, how can I make a cloned copy that has absolutely no residual links to the old design files, so that I can be 100% confident that the new cloned directory is going to be self-contained and free from broken reference errors?

For a single assembly or part it would be a simple case of using the "Pack and Go" feature of solidworks, but how can I reliably do this for multiple assemblies that are themselves cross-linked? I'm worried that I might make a mistake somewhere and not realise it until a year later by which time it would be almost impossible to fix.

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You hinted at the answer in your original question - Pack and Go.

If this were my project, I would create a 'Package Master' top level assembly that contains your 40 assembly files as sub-assemblies. No need to mate them to each other, just have them there contained within the file.

Then use the Pack and Go feature that you're familiar with. I always use the Select/Replace tool to remove the previous 'version number', and update with the latest one, so that you never get in trouble with two different parts having the same filename, and either windows or a user getting confused between these.

Make sure you tick the 'Include Drawings', 'Include Suppressed Components' etc. boxes at the top left of the Pack and Go dialogue according to your needs.

You can delete the 'Package Master' from the target directory once everything has gone through, if you don't need it any more.

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  • $\begingroup$ +1 This sounds promising. I'd need to add each part and then immediately suppress it otherwise my machine would have a hard time loading everything at once. I'll do a trial run with a small project first and then report back in a day or two. Thank you. $\endgroup$
    – user6335
    Commented Apr 25, 2019 at 10:42
  • $\begingroup$ Set it to be in lightweight mode by default before you start! $\endgroup$
    – Jonathan R Swift
    Commented Apr 25, 2019 at 13:24
  • $\begingroup$ This looks like it does the trick, at least on a quick test project I put together. Nice one Jonathan :) $\endgroup$
    – user6335
    Commented Apr 25, 2019 at 14:30
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I would make a copy onto a USB stick then, at best, check that on a separate computer - any broken links should show up.

If you don't have separate computer then a new account may do the same - as long as it does not get access to your user file directory.

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  • $\begingroup$ That is a good way to verify that the method has worked, but it lacks an actual method of performing the cloning process. Also loading, rebuilding and checking nearly 1000 files for small subtle errors will take weeks. $\endgroup$
    – user6335
    Commented Apr 25, 2019 at 8:39
  • $\begingroup$ @Wossname "copy onto a usb"... you can drag & drop or use a command line command ie cp or equivalent. Or you could make a clone of the haddrive onto a new drive - there are several programs that do cloning CCC is one example. depends on which system you use. $\endgroup$
    – Solar Mike
    Commented Apr 25, 2019 at 8:42
  • $\begingroup$ I've had a play around with this idea but unfortunately it's still retaining links to both file and feature level references. Even doing it in the "Solidworks Explorer" does this, I'm not really surprised to be honest, now that I know what the problem is I can't really blame windows for not understanding Solidworks. $\endgroup$
    – user6335
    Commented Apr 25, 2019 at 10:46
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Most operating systems can substitute the path so that after the operation another path looks like another. So from the softwares perspective it is the same path even if it is not. This is a very easy way out as you dont need to change anything at all. How you do this depends a bit how your computer/network is set up.

This said solidworks includes a tool called solidworks explorer that will handle updating file level structure changes. Use that for the moving of files.

Ideally, instead of copying disk level items, you would have let your PDM handle this, as this leaves a link between versions for traceability and other operations. But it sounds like you dont have one and or dont want to use one. In this kind of cases i might be tempted to just set the stff up for a vrsion control system.

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    $\begingroup$ In your first paragraph, you're describing symlinking. For more info on what these are, and an awesome Shell Extension to allow creation of these using a right-click context menu rather than Command Prompt, have a read here:schinagl.priv.at/nt/hardlinkshellext/linkshellextension.html [I am not advocating this as an answer to the original question, but I find this tool useful so thought it worth sharing] $\endgroup$
    – Jonathan R Swift
    Commented Apr 25, 2019 at 10:28

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